optimal clearance ?


Page 1 of 2 12 LastLast
Results 1 to 12 of 14

Thread: optimal clearance ?

  1. #1
    scaring mice @ north pole deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    2338
    Downloads
    0
    Uploads
    0

    Default optimal clearance ?

    hello i would like asking you about how much clearance do you use ...

    on lathe i use 2.5 mm

    on mill i use 5mm; i use more because i am not yet comfortable with the machine ... i worked more on lathes


    i am asking this like is there a minimal value, so the motors to speed up and reach optimal value before tool enters the material ?
    is my 2.5 too low ?
    should i consider a reaction time, for example, of 5 complete revolutions ? or 0.3 seconds ? kindly !

    Similar Threads:
    if you wish to be famous, first you have to succeed
    ... where is Sid ?



  2. #2
    scaring mice @ north pole deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    2338
    Downloads
    0
    Uploads
    0

    Default Re: optimal clearance ?

    my only "clue" is that minimal clearance must allow motors to reach optimal values

    i think that there should be no worries for the "rotary axis" :
    ... lathe :
    ...... S is stared when turret is at safe position
    ...... M is started same as S, or at least when tool is above the fixtures
    ... mill :
    ...... S is stared when tool is at max Z, right after a tool change procedure or
    ...... S is stared at least when tool is above the fixtures
    * this position where rotary axis starts is generally >>> clearance ( much GT clearance ), so no worries here if spindle can accelerate fast



    but what about "linear axis" ? i will check if my minimal clearances are enough for my highest cutting specs :
    ... lathe :
    ...... highest n * f : 2000 x 0.3 = 600 mm/min
    ...... clearance of 2.5 will be "vanished" in 2.5 / 600 * 60 = 0.25 seconds
    ...... note : highest n*f that i used for lathe is 2000x0.6, but this movement did not start with "f 0.6", but with a lower feed "0.2", and feed acceleration was while tool/knife was inside the material; if i would have started with highest feed, than tool may got broken when entering the material; is that "in" & "out" shocks

    ... mill :
    ...... highest n * fz * z : 1200 x 0.12 x 14 = 2016 mm/min
    ...... clearance of 5 will be "vanished" in 5 / 2016 * 60 = 0.15 seconds
    ...... note : i used 8000 x 0.08 x 14 inside aluminium, but i give up later, because parts were not payed well, and is not ok to go on such high rpm's on BT50

    Last edited by deadlykitten; 01-25-2017 at 03:45 AM.
    if you wish to be famous, first you have to succeed
    ... where is Sid ?



  3. #3
    scaring mice @ north pole deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    2338
    Downloads
    0
    Uploads
    0

    Default Re: optimal clearance ?

    so is 0.15 .. 0.25 seconds enough for a linear axis to speed up ? pls shoot me (**) i don't know ...

    if i think of the "load monitor imune time = 0.4 .. 0.8 ", than maybe would be ok to have enough clearance so the tool will enter the material after "imune time"

    Q&A
    1) what if the axis is still accelerating when tool is entering the material ?
    ... if cutting depth is ok, than i guess there is nothing to worry about ...

    2) what if the tool is entering the material before "imune time" ?
    ... then "entering" will not be monitored
    ... (*)

    3) is there a situation where clearance must allow motors to definetly reach optimal domain ?
    ... i think this matters only when surface quality is a must, like machining shiny parts with smooth surface



    ( * ) on mills "tool effort" must be > "limit" for at least 1 second, so this "greater effort minimal duration" of 1 second is actually a greater problem on mill than the idea of this thread; about mill reaction time of 1 second i read inside the manuals, so please, if someone has experience with monitoring on mills, please share if reaction time is really that big

    if a o25 drill goes broken, than :
    ... lathe will stop it after 0.1 seconds, enough to save the insert holder / tool
    ... mill will stop it after 1 second + reaction time; for a cutting spec of 1500 x 0.2 = 300mm/min, in 1 second, tool will travel 5 mm

    ( ** ) don't

    Last edited by deadlykitten; 01-25-2017 at 04:52 AM.
    if you wish to be famous, first you have to succeed
    ... where is Sid ?



  4. #4
    scaring mice @ north pole deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    2338
    Downloads
    0
    Uploads
    0

    Default Re: optimal clearance ?

    hello i found it : optimal distance ( δ ) should allow the "linear" and the "rotary" axis to get in sync :

    δ >= n * f * k / 1000, where :
    ... n * f : cutting specs
    ... k : cnc constant ( see attached image )

    for example, for a 2000o/min * 0.15mm/o : δ >= 2000 * 0.15 * 0.7 / 1000 = 0.21 mm



    on normal turning, when roughing or when finishing with common tolerances, there is no problem if the sync is achieved after the tool entered the material

    this applies also when direction varies, for example when taking a corner : acceleration and deceleration are done inside the material ( where else ? )

    M61 + G96 will boost things a bit also M63 modal + G97 might help a bit at the begining of the toolpath

    acc&decc is inside the material, and things mentioned above only reduce a bit the duration of this phenomen



    optimal clearance matters more when threading, because the f(pitch) is higher

    when threading, it matters before and after the thread, thus the toolpath is bounded between 2 danger zones

    i have a running setup that delivers pitch1.5 at 1000rpm : δ >= 1000 * 1.5 * 0.7 / 1000 = 1.05mm

    on this setup i have low clearances ( attached image )

    at this moment i am glad that i am doing this on an Okuma it may be possible that this setup will fail on another cnc, if sync is delayed kindly !

    Attached Thumbnails Attached Thumbnails optimal clearance ?-01-jpg   optimal clearance ?-02-jpg  
    if you wish to be famous, first you have to succeed
    ... where is Sid ?



  5. #5
    Registered OkumaWiz's Avatar
    Join Date
    Apr 2009
    Location
    United States
    Posts
    1018
    Downloads
    0
    Uploads
    0

    Default Re: optimal clearance ?

    Congrats on finding the chart I was going to tell you about. In most instances the accel doesn't matter, but in cases of threading on a lathe, this becomes very important for getting thread pitch correct with no "lead variation". As you can see, many factors can affect the accel due to variations in ballscrew pitch, motor size, turret mass, head mass, etc. and Okuma provides you with the needed info and the formula to figure out the needed distance to achieve the desired rate. Pretty much all of the Okumas now have high G servos so they can usually hit full rapid within about 12mm as a rule of thumb. That is usually only 1 rev of the ballscrew in most cases. Many competitors will take much longer to reach rate so even with a fast advertised rapid, they may not reach it until it half way across the travel at which point it is almost ready to start slowing down! I believe that the deceleration occurs quicker than the accel since it is being dynamically braked by the motor. I've heard 3 times faster but have not confirmed other than by actual trials where thread decel needed to be short and a good thread was still produced inside of the accel value that was calculated.

    On another note, the Load monitor immune time is set to .4 second which is plenty in nearly all cases. You may need to shorten it in order to monitor such things as peck drilling or threading since the feed motion may not be longer than .4 second in some cases. With a little creative thinking, you can calculate the needed value from your formula.


    I typically use 2mm clearance unless working with castings. As always some adjustments needed for conditions.

    Best regards,

    Experience is what you get just after you needed it.


  6. #6
    scaring mice @ north pole deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    2338
    Downloads
    0
    Uploads
    0

    Default Re: optimal clearance ?

    hello mr Wizard good to see you

    Pretty much all of the Okumas now have high G servos so they can usually hit full rapid within about 12mm as a rule of thumb. That is usually only 1 rev of the ballscrew in most cases
    that's definetly mr Wizards experience

    I believe that the deceleration occurs quicker than the accel since it is being dynamically braked by the motor. I've heard 3 times faster but have not confirmed other than by actual trials where thread decel needed to be short and a good thread was still produced inside of the accel value that was calculated.
    yup, the hiG diagram is not symetric, and i really don't like when i have shocks durings turning, but in the end it delivers a good thread with low front/back clearances

    like how the "k = cnc constant" varies with machine type, also "acceleration" times varies with machine type : somehow is the same thing, a heavy turret will be slower than a light one, but still, the numbers are good, and i guess that anyone who delivered a thread with low clearances has saw that

    With a little creative thinking, you can calculate the needed value from your formula. I typically use 2mm clearance unless working with castings
    i use 5 and dynamic indexing after finding this chart, i will calculate those distances for my specs, and maybe i will also reduce this clearance

    On another note, the Load monitor immune time is set to .4 second which is plenty in nearly all cases. You may need to shorten it in order to monitor such things as peck drilling or threading since the feed motion may not be longer than .4 second in some cases
    now i don't monitor threads, since the operator is near the lathe

    and drilling with circa 0.4 + LM is not common
    ... if tool is little, it can not be sensed
    ... if tool is big, and cutting is for 0.4 seconds, than is a rare situation
    ... if tool is normal, than is the case when you try to cut deeper, chips dont go out, etc ...

    ...in some cases
    about particular cases, i would like to tell you that i monitor cutting inserts ( generally width=3 ) with caution

    the cnc can not feel this insert, but it can feel if the insert is broken and the holder is making contact with the part

    thus a good limit may save your holder when the operator is not paying atention : well, is a bit hard to react, especially if material has a tough crust

    so far i saved the holder many times .... and i trashed many holders before

    so during a setup i always have a warning on the cnc scrren, because of the limits but it works

    all the best

    if you wish to be famous, first you have to succeed
    ... where is Sid ?



  7. #7
    scaring mice @ north pole deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    2338
    Downloads
    0
    Uploads
    0

    Default Re: optimal clearance ?

    those distances may be even smaller in reality, if guys from Okuma have used safety coeficients when calculating the values for K

    when LM=100, you can still go ...

    LM is there for a reference, for safety, but those cncs can be pushed until tool stops inside the material, and i don't think that someone had such kind of problems

    if you wish to be famous, first you have to succeed
    ... where is Sid ?



  8. #8
    scaring mice @ north pole deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    2338
    Downloads
    0
    Uploads
    0

    Default Re: optimal clearance ?

    I typically use 2mm clearance unless working with castings. As always some adjustments needed for conditions
    i just scanned my running programs ; generaly i use :
    ... 5mm when knife is in front of the part
    ... 2.5mm when live tool is in front of the part
    ... 2mm when tool is coming from above, thus feed direction is on X

    i never thougth to make all equal i was feeling comfortable ... thanks again for the sugestion

    if you wish to be famous, first you have to succeed
    ... where is Sid ?



  9. #9
    scaring mice @ north pole deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    2338
    Downloads
    0
    Uploads
    0

    Default Re: optimal clearance ?

    hello there is a "thing" when using low clearances, and i am afraid not to begin cutting at an increased diff value ...

    pls consider that the part is at Z0, and there is a Z_clearance=2.5

    Code:
        NOEX LVOX = 24424.689 LVOZ = 15678.463 ( encoders origins )
    
        turret @ safe pos
        G00 X50 Z2.5
        M331 ( stops the buffer, so to avoid the case when V1 & V2 are calculated too soon )
        NOEX V1 = VAPAX - LVOX - VETFX         - 50  ( delivers actual_x - program_x )
        NOEX V2 = VAPAZ - LVOZ - VETFZ - VSZOZ - 2.5 ( idem for z )
        G01 Z-whatever   
    if " rapids are high " & " droop control is off ", V1 can be 7mm, and V2 can be 15mm

    when the feeding movement begins, will diff become 0 ( or close to it ) right at the moment when execution begins ( attached image "case 3" ), or somewhere along the way ( attached image "case 2" ) ?

    i need a way to be sure, or " cnc fail army " ... kindly



    V1 = 9.388 when M331 is not there
    V1 = 7.133 when M331 is used once
    V1 = 0.368 when M331x6
    V1 = 0.001 when M331x18; definetly rocket science

    Attached Thumbnails Attached Thumbnails optimal clearance ?-01-jpg   optimal clearance ?-02-jpg  
    Last edited by deadlykitten; 05-07-2018 at 01:22 PM.
    if you wish to be famous, first you have to succeed
    ... where is Sid ?



  10. #10
    scaring mice @ north pole deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    2338
    Downloads
    0
    Uploads
    0

    Default Re: optimal clearance ?

    hello when indexing the turret at low clearances, like <2.5mm, i was afraid that a collision may appear : if i run the code in step-by-step, then all seems ok, but if i run it continuous, things are moving too fast and i can no longer observe what is going on

    i needed to be sure that a colision does not occur, without increasing the clearance distance

    pls consider this example :
    ... turret rotation speed @ 100%
    ... rapids 100%
    ... turret is moving down ( towards X- ) at index position
    ... a long drill is indexing at X0 Z1.25mm and after that it is going in rapid inside the part ( after indexing, rapid is executed only on Z axis )

    in this conditions, will the tool interfere with the part ?





    to handle this case, thus to index with low clearances, and without being affraid of a collision, i started using droop control :

    Code:
        turret at safe position
        NOEX VINPX = 0.4
        NOEX VINPZ = 0.4
        NOEX G65
        T M66 S M08 G00 IP M63
        NOEX G64
        linear movement : rapid or feed
    this code delivers droop control only for a single joint-point; thus the "linear movement" is executed only after a droop control check

    if you replace NOEX G65 with G65, than downtime will appear, because also turret safe position will be subject to droop control check

    all is ok, as long as VINP* < clearance





    code shared in this post is a simple example of how to use this technique; real codes that i use, especially for long setups, are a bit more complex, but this is a story for another time

    if you wish to be famous, first you have to succeed
    ... where is Sid ?



  11. #11
    Registered OkumaWiz's Avatar
    Join Date
    Apr 2009
    Location
    United States
    Posts
    1018
    Downloads
    0
    Uploads
    0

    Default Re: optimal clearance ?

    You waste more time....

    Consider that it takes 3/4 of a second to unclamp the turret. I that same time you can rapid away from the part so you have now worries about indexing.

    It takes another 3/ of a second to clamp so you can rapid back to the part while it clamps.

    You need no goofy code that only you understand and you save NO time by going through all the extra steps.

    KISS is the best rule.

    It appears that you are mostly talking to yourself in this post...

    Best regards,

    Experience is what you get just after you needed it.


  12. #12
    scaring mice @ north pole deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    2338
    Downloads
    0
    Uploads
    0

    Default Re: optimal clearance ?

    hello mr Wizard

    ... sometimes the safe position is reached, and the turret is still unclamping
    ... sometimes there is no need to rapid back to the part
    ... clearances are pretty low
    ... there are time charts, so to analyze the amount of time gain
    + others





    i have a folder, called " hollywood ", inside which i have 3 short movies, with setups that are using dynamic indexing

    next update should handle " middle index function " and " combi holders "

    in that moment, i will share the videos, because only the code, is not interesting the video is more communicative, more self-explanatory

    i don't rush, i need to be sure, or i will crash the machine





    i helped a guy with some parts; i put the dynamic indexing ( because setup would last a couple of days ), and i left from his shop without worries / kindly

    Last edited by deadlykitten; 07-13-2018 at 04:39 AM.
    if you wish to be famous, first you have to succeed
    ... where is Sid ?



Page 1 of 2 12 LastLast

Tags for this Thread

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •  


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

optimal clearance ?

optimal clearance ?